Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 

custom pad problem.

Hi All,

 

Just started using Multisim and Ultiboard and I like it so far. 

 

I'm making a footprint for a Luxeon Rebel LED and I'm having a problem with the thermal pad. I was able to import most of the footprint from an Orcad Library that I found on the manufacturer's website. It didn't include a solder mask for the thermal pad though.

 

The pad is a goofy shape which makes it tough to draw in Ultiboard. I have a DXF file for the part and was able to import the thermal pad shape into ultiboard, but it is just an outline of the pad, not solid. Is there an easy way to fill it in?

 

Thanks,

Jeff

 

 

 

 

0 Kudos
Message 1 of 2
(4,853 Views)

JZimmerman ,

 

Hopefully this helps...  I think this will benefit others wanting to create parts with custom pads or thermal shapes for inclusion into a custom part.  It is relatively detailed so you can find the detailed notes and design files I used attached...  Here is a summarized version...

 

 Note: The Ultiboard PowerPro allows you to do import/export to DXF.   Custom pads can be created from Ultiboard Full using a filled polygon and using the datasheet, however the DXF import technique will be more precise.

 

1. Start by importing the DXF file into an empty design.  Remove everything except the pad outlines.  The problem with this DXF is that the PADs are not filled... 

 **Creating the Custom PADS** 

2. There are a few ways to do this, but the most useful and easiest technique is to zoom into these pad outlines and take a screen shot and paste into MS Paint.   Use the fill feature to create a black/white bmp file (pad should be white, background should be black).  Save each pad with its own b/w bmp file...

3. Back in Ultiboard, copy the reference DXF pad outlines and in the Database Manager create a new Custom Pad Shape and paste the reference pad outlines here.  Use the Place -> Picture function to place the B/W pad outline over the pad oultines and resize as needed to get the exact shape.   You can get these exact since the referenced outline data is coming from the original DXF file.  Delete the reference, leaving the BMP data and save the pad shapes separately for each unique pad shape (in these case all 3 are unique)..

**Creating the Custom Footprint**

4. Next again copy the reference DXF pad outlines and in the Database Manager create a new PCB Part (i.e. footprint) and again paste the reference pad outlines here.   Use the Place -> Pin to add the 3 custom pad shapes to the design (best to do it in order 1=Cathode, 2=Anode, 3=Thermal).   Use rectangles, circles to add any other dimensional or shape information to the footprint.

5. Finally go into Multisim and create the symbol and attach to the footprint (note you'll need to remember the exact Ultiboard shape name you created as this needs to be identified in Multisim).

6.  You can also use this technique to add and align the thermal VIAs and the white reflective area to the silkscreen layer.

 

The attachment includes additional notes, the Ultiboard files with footprint shape and added thermal relief vias, and a reference schematic with an added virtual LED model.

 

Regards,

Patrick Noonan
Business Development Manager
National Instruments - Electronics Workbench Group
50 Market St. 1-A
S. Portland, ME 04106
Email: patrick.noonan@ni.com
Tel. (207) 892-9130
Fax. (207) 892-9508 

0 Kudos
Message 2 of 2
(4,793 Views)